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Using External References


Im new to Catia, only using it for a day or two.

So say that I have multiple other files with master geometry that I want to use, planes, lines, axis, etc. How to I create a separate part and use some of those references in the new part?



Super Moderator
(3 part answer)

One way to use reference geomety is with CCP links (Copy & Paste).

1. Open both CATParts in two, separate windows
2. In the parent window, Copy the geometry (sketch, plane, surface, body, etc) from the "pointed document"
3. Switch to the child window, Paste Special + As Result With Link to add the referenced geometry with a link.

EDIT + LINKS will show the referenced features with a CCP type of link.
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Super Moderator
(part 2)

Another way to create referenced geometry is with IMPORT links:

1. create an Assembly and insert the parent and child parts into this assembly (or use an existing Assembly containing both parts). The assembly is the "context"
2. with the Assembly and the parts open in one window, double click on the child part to make it active. (this is the part receiving the referenced geometry. The active part will have a blue background in the tree, and the Part Design workbench should be active even though an assembly of parts is being displayed.
3. create/modify features as normal, but select referenced geometry in the parent part as required. This will make reference geometry that is linked back to the "pointed document"

EDIT + LINKS will show the referenced geometry as an IMPORT link, and the parent assembly as a CONTEXT link.

The disadvantage of using this method is that the Context link will cause the assembly and all of it's parts to be loaded into CATIA when the the part with the link is opened.
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Super Moderator
(part 3 - some tips and suggestions on either method)

A. Using referenced features has many advantages and provides for efficient modeling practices. Many companies use CATIA this way. Making a small change to the parent document will be passed down to all the children documents.

B. It is common practice to put all the "master" geometry in one (or more) CATParts files, and then make links from those parts. These files are sometimes called "skeletons" because they only contain the master geometry and seldom have solid geometry.

C. Links should always be mono-directional (parent to child). Avoid bi-directional links (A to B, and B to A).

D. It is strongly recommended to Publish the features in the Parent document, and link to the Publications. This will make it much easier to replace parts/features.

e. Care should be taken to maintain good links between CATIA files. Always use File + Save Management to save modified files. Never rename or move files with links - instead, use File + Save Mangement + SAVE AS to rename and move files.
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